OS-T: 6080 Sine Sweep Fatigue Analysis (SN Damage)

This tutorial provides an overview of fatigue life of structures under Sinusoidal Loading,

The following file found in the optistruct.zip file is needed to perform this tutorial. Refer to Access the Model Files.

bracket-frf.fem

A copy of the model file used in this tutorial is available on <install_directory>/tutorials/hwsolvers/optistruct.

A bracket tested for frequency response analysis is utilized to perform the Sine Sweep Fatigue Analysis. The model is already setup for the FRF analysis, an additional loadstep for SN-Fatigue Calculation is created in this tutorial. The FRF subcase will be utilized for the fatigue calculation, and a TABLED card scaling the same.

Note: The sweep parameters are currently supported by editing the .fem deck generated, which is explained in this tutorial.

Launch HyperMesh and Set the OptiStruct User Profile

Launch HyperMesh.
The User Profile dialog opens.
Select OptiStruct and click OK.
This loads the user profile. It includes the appropriate template, macro menu, and import reader, paring down the functionality of HyperMesh to what is relevant for generating models for OptiStruct.

Import the Model

Click File > Import > Solver Deck.
An Import tab is added to your tab menu.
For the File type, select OptiStruct.
Select the Files icon .
A Select OptiStruct file browser opens.
Select the bracket_frf.fem file you saved to your working directory from the optistruct.zip file. Refer to Access the Model Files.
Click Open.
Click Import, then click Close to close the Import tab.

The outline of the Fatigue Analysis setup to be achieved in the following steps.
Figure 2. Fatigue Setup Sine Sweep – SN Damage

Set Up the Model

Create TABLED1 Load Collector

In the Model Browser, right-click and select Create > Load Collector.
For Name, enter tabled-fat.
For Card Image, select TABLED1 from the drop-down menu.
Set XAXIS and YAXIS to LINEAR.
For TABLED1_NUM, enter a value of 2 and press Enter.
Click the Table icon below TABLED1_NUM and enter the values in the pop-out window, as shown below.

Figure 3. TABLED1 Card
Click Close.
The load collector TABLED1 that defines the time history of the loading has been created.

Define FATLOAD Load Collector

The model has a Frequency Response loadstep defined, which is used to define the FATLOAD.

In the Model Browser, right-click and select Create > Load Collector.
For Name, enter fatload_fat.
For Card Image, select FATLOAD.
Select the option for TID INTEGER.
Set the TID value as the load collector ID of tabled-fat (8 in this tutorial).
For LCID(load case ID), select 03_frf from the list of load steps.

Note: TABFAT and scaling parameters are not required for this calculation.
Select the Option for SWEEP and define the sine sweep parameters via SR (sweep rate) and SRUNIT (sweep rate unit) fields.

Figure 4. FATLOAD with LCID and SWEEP Parameters

Define FATEVNT Load Collector

Create a random response event for the FATLOAD_RAND created.

In the Model Browser, right-click and select Create > Load Collector.
For Name, enter fatevent-fat.
For Card Image, select FATEVNT.
For FATEVNT_NUM_FLOAD, enter 1.
Select fatload-fat for FLOAD in the Loadcol field.

Define FATSEQ Load Collector

In the Model Browser, right-click and select Create > Load Collector.
For Name, enter fatseq-fat.
For Card Image, select FATSEQ.
For FATSEQ_NUM enter 1, as 1 FATEVENT has been created.
For FID (Fatigue Event Definition), select fatevent-fat and N as 1.

Figure 5. FATSEQ showing fatevent-fat created

Defining the sequence of events for the fatigue analysis is completed. The Fatigue parameters are defined next.

Define Fatigue Parameters

In the Model Browser, right-click and select Create > Load Collector.
For Name, enter fatparm-fat.
For Card Image, select FATPARM.
Verify TYPE is set to SN.
Set STRESS COMBINE to VONMISES.
Set STRESSU to MPA (Stress Units).
Set SURVCERT in CERTNTY to 0.9.
Select the SWEEP option and define NF=30.

Figure 6. FATPARM with SWEEP Parameters

Define Fatigue Material Properties

The material curve for the fatigue analysis can be defined on the MAT1 card.

In the Model Browser, click on the MAT1 material.
The Entity Editor opens.
In the Entity Editor, set MATFAT to SN.
Set UTS (ultimate tensile stress) to 340.0.
Set YS (yield strength) to 180.0.
For the SN curve set (these values should be obtained from the material's SN curve):

SRI1

936.0

B1

-0.161907

NC1

1e20

FL

1.0

SE

1.0

Define PFAT Load Collector

In the Model Browser, right-click and select Create > Load Collector.
For Name, enter pfat-fat.
For Card Image, select PFAT.
Set LAYER to WORST.
Set FINISH to NONE.
Set TRTMENT to NONE.
Set Kf to 1.0.

Define FATDEF Load Collector

In the Model Browser, right-click and select Create > Load Collector.
For Name, enter fatdef-fat.
Set the Card Image to FATDEF.
Activate PTYPE and PSHELL in the Entity Editor.
Edit FATDEF_PSOLID_NUMIDS to 1.
Select new_bracket for PID and pfat-fat for PFATID.

Define the Fatigue Load Step

In the Model Browser, right-click and select Create > Load Step.
For Name, enter 04-Fatigue.
Set the Analysis type to fatigue.
For FATDEF, select fatdef-fat.
For FATPARM, select fatparm-fat.
For FATSEQ, select fatseq-fat.

Submit the Job

From the Analysis page, enter the OptiStruct panel.
Click save as following the input file field.
The Save As dialog opens.
For File name, enter the name bracket-frf.fem.
Click Save.
Click OptiStruct to submit the analysis.

Review the Results

From the OptiStruct panel, click HyperView.
HyperView is launched and the results are loaded. A message window appears to inform of the successful model and result files loading into HyperView.
Go to the Results tab.
In the Results tab, select Subcase 4 (04-Fatigue) from the subcase field.
On the Results toolbar, click to open the Contour panel.
Set Result type to Damage and click on Apply to contour the elements.

Figure 7. Damage Contour Plot